I am writing Abaqus USDFLD to change my Young's Modulus after strain crosses the value of 0.035 and start deleting elements when strain value crosses 0.05 in a heterogeneous model (composed of two different sections).
I am using linear degradation; (1-D)*E where D goes from 0 to 1 as strain goes from 0.035 to 0.05.
See the image below, and I want that degradation to follow the linear curve.
So, my problem is how do I infer the young's modulus (E) and which section I am at when I use the GETVRM subroutine to get values at the integration point? I have checked the Abaqus documentation but couldn't find the method to get E at the integration points. Is there any alternative way to accomplish this?
And I am assuming we need to supply the same subroutine file (.for) for all the material, which gives rise to this issue, and I am unsure how to supply different subroutine files for all the different sections we have. Is this possible?
Hi Ayush,
The Abaqus Documentation for USDFLD provides a worked example of the use of a field variable to reduce Youngs modulus as the material strains. This would be a good starting point.
The USDFLD routine argument list contains CMNAME which is the "User-specified material name". I assume that you could test this name in the user routine and specify different field variable options for each of the materials in your model. In other words, you have one USDFLD routine with a test in it to determine the material associated with each region in your model.
Does that help?
Regards,
Simon
Simon Smith sir, I am pretty new to this. Please answer this doubt of mine; if I write the value of FIELD as 1 in the material definition see image below, can I access the E value by using FIELD(1) in the subroutine script? If so, then I can easily change this to FIELD(1) = FIELD(1)* (1-D). I am assuming here that we can access the value of E by FIELD(1) as they have been alias to one another. Is this how Abaqus works?
Hi Ayush,
An extract below shows part of the worked example from the Abaqus documentation. Field variable 1 varies from 0 to 0.04. The Youngs modulus is 2000 when the field variable is 0.0 and 1000 when the field variable is 0.04. The number between 0.0 and 0.04 is the "absolute value of current strain". So, you use USDFLD to find the value of the strain of interest and equate FIELD(1) to this value of strain. Abaqus will use the table below and the value of FIELD(1) to calculate the current value of E. This means you do the E*(1 - D) calculation and create the required numbers of rows in the "Edit Material" box.
Regards,
Simon
*MATERIAL, NAME=ELASTIC
*ELASTIC, DEPENDENCIES=1
** Table of modulus values decreasing as a function
** of field variable 1.
2000., 0.3, 0., 0.00
1500., 0.3, 0., 0.01
1200., 0.3, 0., 0.02
1000., 0.3, 0., 0.04
Simon Smith sir, say yes if I get it right,
I precalculate the values of E at various strain values and fill the "Elastic" properties with the E values and their corresponding strain values in the Field 1 column. Then when I calculate the strain values and do field(1) = stain_value, Abaqus will pick the corresponding E values I just defined in the "Elastic" properties table. And where Abaqus can't find the exact value for E at some strain, will it interpolate?
Simon Smith, sir, I have coded the subroutine successfully, but now I have convergence issues. My program doesn't run till the end of the step. I have tried various things like lower seed length, non-linear geometry, but it didn't help.
Please help me with this. I have attached the code for your reference below.
Hi Ayush,
Your routine looks good. Are you loading your model via a force of a displacement?
Simon (PS please call me Simon)
Simon Smith, that's too humble of you, but I am young enough qualifying me saying you, Sir.
I am applying a displacement boundary condition at the top surface of the cube (see fig. attached)
Hi Ayush,
I suggest you add a Y constraint over the whole of the bottom of the cube instead of just the edges. I also suggest you add two X constraints at different points on the Z axis and one Z constraint somewhere on the X axis.
And please make an exception and call me Simon even though I am over the hill.
Regards,
Simon
If you are not generally familiar with subroutines, you can find some details about subroutine in this article:
https://caeassistant.com/blog/start-writing-subroutine-in-abaqus/
You can find more details about USDFLD and VUSDFLD with different practical examples in the following link. You can find step-by-step video training in this training.
https://caeassistant.com/product/usdfld/
- Badges
- Science topic
- Similar topics
- Biological Science
- Physiology
- Physiological Processes
- Stress